# What is the maximum signal frequency SPICE can handle ?

Started by March 22, 2012
```Could some electronics guru tell me what
is the maximum signal frequency that the
SPICE can handle ? I have experimented
with a simple low pass LC filter and found
that the maximum input frequency that it
can handle (before the output looks like
junk) is 1 THz (10^12 Hz) even when the
cutoff has been set to 150 THz. What are

```
```On 2012-03-22, dakupoto@gmail.com <dakupoto@gmail.com> wrote:
> Could some electronics guru tell me what
> is the maximum signal frequency that the
> SPICE can handle ?

blue perhaps.

how good are your parts models?

--
&#9858;&#9859; 100% natural
```
```On 2012-03-22, dakupoto@gmail.com <dakupoto@gmail.com> wrote:
> Could some electronics guru tell me what
> is the maximum signal frequency that the
> SPICE can handle ?

That depends on how low you can set the step size and how well your
models match real parts.

There's a theoretical limit where you run out of mantissa in the
floating point but you'd be simulating gamma ray frequencies before
you hit that limit.

I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what
appeared to be consistent results.

At the end of the day it's just arithmentic.

--
&#9858;&#9859; 100% natural
```
```On Mar 22, 5:30=C2=A0am, Jasen Betts <ja...@xnet.co.nz> wrote:
> On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote:
>
> > Could some electronics guru tell me what
> > is the maximum signal frequency that the
> > SPICE can handle ?
>
> That depends on how low you can set the step size and how well your
> models match real parts.
>
> There's a theoretical limit where you run out of mantissa in the
> floating point but you'd be simulating gamma ray frequencies before
> you hit that limit.
>
> I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what
> appeared to be consistent results.
>
> At the end of the day it's just arithmentic.
>
> --
> =E2=9A=82=E2=9A=83 100% natural

YES! separate math limit from simulation effectiveness limit.

IME, for discrete components at around 10MHz, PSpice seems to no
longer represent reality.  I've always attributed that to the
'weakness' in the modeling, but never bothered to pursue further.
Inside components, translate that to SMALL geometry, at around 100MHz.

Mathematically I constantly use to beyond 1GHz, however, more for
'learning' what's going on than 'describing' what's going on.

At 1+ THz, EVERYTHING must be acting like a radiating, transmission
line. Can't imagine the complexity of a useful model. Even the
wavefronts through conduction must have some effects, right? Be like
trying to model the acoustics of a concert hall with all that wave/
reflections, etc.

```
```Robert Macy wrote:
>
> On Mar 22, 5:30&#2013265922; am, Jasen Betts <ja...@xnet.co.nz> wrote:
> > On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote:
> >
> > > Could some electronics guru tell me what
> > > is the maximum signal frequency that the
> > > SPICE can handle ?
> >
> > That depends on how low you can set the step size and how well your
> > models match real parts.
> >
> > There's a theoretical limit where you run out of mantissa in the
> > floating point but you'd be simulating gamma ray frequencies before
> > you hit that limit.
> >
> > I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what
> > appeared to be consistent results.
> >
> > At the end of the day it's just arithmentic.
> >
> > --
> > &#9858;&#9859; 100% natural
>
> YES! separate math limit from simulation effectiveness limit.
>
> IME, for discrete components at around 10MHz, PSpice seems to no
> longer represent reality.  I've always attributed that to the
> 'weakness' in the modeling, but never bothered to pursue further.
> Inside components, translate that to SMALL geometry, at around 100MHz.
>
> Mathematically I constantly use to beyond 1GHz, however, more for
> 'learning' what's going on than 'describing' what's going on.
>
> At 1+ THz, EVERYTHING must be acting like a radiating, transmission
> line. Can't imagine the complexity of a useful model. Even the
> wavefronts through conduction must have some effects, right? Be like
> trying to model the acoustics of a concert hall with all that wave/
> reflections, etc.

Below about 10 THz, the method of moments (MOM) works okay.  Above
there, material dispersion and limited conductivity make full-wave
simulations de rigueur--FEM or FDTD, usually.

The conductivity limit comes in because the effective dielectric
constant of a normal conductor is

epsilon = epsilon.re + j sigma/omega

so conductors look steadily less conductive as the frequency goes up.
Antenna simulations using MOM at 28 THz (CO2 laser territory) look
vaguely like the fullwave ones, and vaguely like the experiments, but if
you go any higher, all resemblance is lost.  My 200 THz stuff was all
fullwave.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC
Optics, Electro-optics, Photonics, Analog Electronics

Briarcliff Manor NY 10510
845-480-2058

hobbs at electrooptical dot net
http://electrooptical.net
```
```On Mar 22, 7:50=C2=A0pm, Phil Hobbs
<pcdhSpamMeSensel...@electrooptical.net> wrote:
> Robert Macy wrote:
>
> > On Mar 22, 5:30=C3=82 am, Jasen Betts <ja...@xnet.co.nz> wrote:
> > > On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote:
>
> > > > Could some electronics guru tell me what
> > > > is the maximum signal frequency that the
> > > > SPICE can handle ?
>
> > > That depends on how low you can set the step size and how well your
> > > models match real parts.
>
> > > There's a theoretical limit where you run out of mantissa in the
> > > floating point but you'd be simulating gamma ray frequencies before
> > > you hit that limit.
>
> > > I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave wh=
at
> > > appeared to be consistent results.
>
> > > At the end of the day it's just arithmentic.
>
> > > --
> > > =C3=A2=C5=A1=E2=80=9A=C3=A2=C5=A1=C6=92 100% natural
>
> > YES! separate math limit from simulation effectiveness limit.
>
> > IME, for discrete components at around 10MHz, PSpice seems to no
> > longer represent reality. =C2=A0I've always attributed that to the
> > 'weakness' in the modeling, but never bothered to pursue further.
> > Inside components, translate that to SMALL geometry, at around 100MHz.
>
> > Mathematically I constantly use to beyond 1GHz, however, more for
> > 'learning' what's going on than 'describing' what's going on.
>
> > At 1+ THz, EVERYTHING must be acting like a radiating, transmission
> > line. Can't imagine the complexity of a useful model. Even the
> > wavefronts through conduction must have some effects, right? Be like
> > trying to model the acoustics of a concert hall with all that wave/
> > reflections, etc.
>
> Below about 10 THz, the method of moments (MOM) works okay. =C2=A0Above
> there, material dispersion and limited conductivity make full-wave
> simulations de rigueur--FEM or FDTD, usually.
>
> The conductivity limit comes in because the effective dielectric
> constant of a normal conductor is
>
> epsilon =3D epsilon.re + j sigma/omega
>
> so conductors look steadily less conductive as the frequency goes up.
> Antenna simulations using MOM at 28 THz (CO2 laser territory) look
> vaguely like the fullwave ones, and vaguely like the experiments, but if
> you go any higher, all resemblance is lost. =C2=A0My 200 THz stuff was al=
l
> fullwave.
>
> Cheers
>
> Phil Hobbs
>
> --
> Dr Philip C D Hobbs
> Principal Consultant
> ElectroOptical Innovations LLC
> Optics, Electro-optics, Photonics, Analog Electronics
>
> 160 North State Road #203
> Briarcliff Manor NY 10510
> 845-480-2058
>
> hobbs at electrooptical dot nethttp://electrooptical.net

spice small documentary

www.commitmentiseverything.com/monkeyman.html?utm_source=3D554261

www.commitmentiseverything.com/moochwala.html?utm_source=3D554261
```
```On Thu, 22 Mar 2012 07:31:12 -0700 (PDT), Robert Macy
<robert.a.macy@gmail.com> wrote:

>On Mar 22, 5:30&#2013266080;am, Jasen Betts <ja...@xnet.co.nz> wrote:
>> On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote:
>>
>> > Could some electronics guru tell me what
>> > is the maximum signal frequency that the
>> > SPICE can handle ?
>>
>> That depends on how low you can set the step size and how well your
>> models match real parts.
>>
>> There's a theoretical limit where you run out of mantissa in the
>> floating point but you'd be simulating gamma ray frequencies before
>> you hit that limit.
>>
>> I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave what
>> appeared to be consistent results.
>>
>> At the end of the day it's just arithmentic.
>>
>> --
>> ?? 100% natural
>
>YES! separate math limit from simulation effectiveness limit.
>
>IME, for discrete components at around 10MHz, PSpice seems to no
>longer represent reality.

I have used PSpice to model RF stages at 5GHZ, no problem.  If you
don't set a "Maximum Time-step" small enough (my rule-of-thumb is 1/32
of the period of the highest frequency... or smaller), you will get a
jagged sampling output.

>I've always attributed that to the
>'weakness' in the modeling, but never bothered to pursue further.

That might be with behaviorally-modeled devices.

>Inside components, translate that to SMALL geometry, at around 100MHz.
>
>Mathematically I constantly use to beyond 1GHz, however, more for
>'learning' what's going on than 'describing' what's going on.
>
>At 1+ THz, EVERYTHING must be acting like a radiating, transmission
>line. Can't imagine the complexity of a useful model. Even the
>wavefronts through conduction must have some effects, right? Be like
>trying to model the acoustics of a concert hall with all that wave/
>reflections, etc.
>

Finite element analysis?

...Jim Thompson
--
| James E.Thompson, CTO                            |    mens     |
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    |
| Phoenix, Arizona  85048    Skype: Contacts Only  |             |
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  |
| E-mail Icon at http://www.analog-innovations.com |    1962     |

I love to cook with wine.     Sometimes I even put it in the food.
```
```On Wed, 21 Mar 2012 23:23:24 -0700 (PDT), dakupoto@gmail.com wrote:

>Could some electronics guru tell me what
>is the maximum signal frequency that the
>SPICE can handle ? I have experimented
>with a simple low pass LC filter and found
>that the maximum input frequency that it
>can handle (before the output looks like
>junk) is 1 THz (10^12 Hz) even when the
>cutoff has been set to 150 THz. What are
>

There should be lots of floating-point range to get to THz. There are
a few Spice parameters that might matter. Minimum time step is one. LT
Spice has "chgtol" and "cshunt" and "cshuntintern" that will matter at
super speeds, possibly others. There is a "minimum inductance damping"
thing, too.

The default Spice is probably optimized/compromised for speed and
convergence with practical circuit values and speeds. After all, you
can't really make a 150 THz LC filter.

--

John Larkin, President
Highland Technology, Inc

jlarkin at highlandtechnology dot com
http://www.highlandtechnology.com

Precision electronic instrumentation
Picosecond-resolution Digital Delay and Pulse generators
Custom laser controllers
Photonics and fiberoptic TTL data links
VME thermocouple, LVDT, synchro   acquisition and simulation
```
```On 22 Mar., 16:47, Jim Thompson <To-Email-Use-The-Envelope-I...@On-My-
Web-Site.com> wrote:
> On Thu, 22 Mar 2012 07:31:12 -0700 (PDT), Robert Macy
>
>
>
>
>
>
>
>
>
> <robert.a.m...@gmail.com> wrote:
> >On Mar 22, 5:30=A0am, Jasen Betts <ja...@xnet.co.nz> wrote:
> >> On 2012-03-22, dakup...@gmail.com <dakup...@gmail.com> wrote:
>
> >> > Could some electronics guru tell me what
> >> > is the maximum signal frequency that the
> >> > SPICE can handle ?
>
> >> That depends on how low you can set the step size and how well your
> >> models match real parts.
>
> >> There's a theoretical limit where you run out of mantissa in the
> >> floating point but you'd be simulating gamma ray frequencies before
> >> you hit that limit.
>
> >> I ran a fimple LPF sim in ltspice with 10THz sine wave and it gave wha=
t
> >> appeared to be consistent results.
>
> >> At the end of the day it's just arithmentic.
>
> >> --
> >> ?? 100% natural
>
> >YES! separate math limit from simulation effectiveness limit.
>
> >IME, for discrete components at around 10MHz, PSpice seems to no
> >longer represent reality.
>
> I have used PSpice to model RF stages at 5GHZ, no problem. =A0If you
> don't set a "Maximum Time-step" small enough (my rule-of-thumb is 1/32
> of the period of the highest frequency... or smaller), you will get a
> jagged sampling output.
>

all spice knows is time steps and equations

it doesn't really know the physical concept of frequency

-Lasse

```